That's a puzzle!I made an attempt a different way, but did not quite get there. Had fun trying.

1. Made a simulated sheet metal part using standard intellishapes (not using sheetmetal tools) just to get geometry to pull from. 2. Created thicken shape part from outer surface geometry.3. Then created flat pattern from surfaces to see how close it looked unfolded.

I got some little joggles in flat at the bend line, but heck it could tell me where to bend it. Now back to work!

Can't see a much better way than what you did. A long time ago I, and others, asked for a way to model sheetmetal from in the flat state. In other words, take a flat piece of stock, add a bend line across the surface, just like you want to do, and then have the sheetmetal bend across the bend line that was drawn when in the flat state. I have had many tapered parts I needed to make, and this feature would have been very valuable and powerful in that case. I'll poke around as time allows to see what can be done.

Would anyone have an effective way to bend the corner of a piece of steel as shown in the image?

This may help, late, but better late than never;

1) Create the base plate, in this case 5mm plate 100 x 100 and create a vertex chamfer in one corner, say 60mm

2) Add a normal bend at opposite corner

3) Perform an "Add Mitre"using the opposing bend and place it on the vertex chamfer cut line

4) The tricky part. Select the bend at intellishape level, select relief mode and change the reliefs both to 'Closed' - 'Top' and the values must represent the inside radius of the bend, plus the material thickness PLUS whatever the hypotenuse of the K factor is for an right angle triangle- in this case K factor is .33, therefore the hypotenuse of a .33 right angle triangle ( two side equal ) would be 0.46. This example then makes the relief to be 10 ( 5 + 5 ) plus 0.46

5) Extend the bend higher than what the next vertex chamfer cuts will be and perform vertex chamfer on one side, using the bend line as finish point

6) Do the same on the other side

7) Kill the opposing bend

8) Unfold - result should be a perfectly square ( or oblong as the case may be ) piece of metal just like you'd have if you'd drawn a 45 degree line across the metal piece and stuck it in a press brake.

The enlightening points for me that I learned from Jonas' methods were;

1) You can edit the shape of a sheetmetal part by selecting the ,Sheet Metal Part xxx' in the Scene tree, expand, RMB on 'Stock' and select Edi cross section.

2) Custom profile is an extremely versatile tool which can be used to manipulate shapes around the outside of a part as well as inside( I ad previously thought that 'custom profile' acted purely like a hole in that its perimeter had to be within the bounds of the part - not so)